Video summary
The video demonstrates how to model a chess bishop in SolidWorks, noting that this specific design differs significantly from traditional bishops which typically feature taller heads. Instead of using complex ellipsoids for the head, the tutorial simplifies the geometry by utilizing spheres to make the example more approachable for learners. Although the initial view of the part's dimensions and arcs can appear intimidating due to their complexity, the narrator explains that geometrically speaking, the entire shape is constructed from just five circles (arcs) and a few straight lines. The modeling process relies primarily on two main features: a revolution feature created by sketching half of the cross-section relative to an axis of revolution, followed by a linear cut extruded through the part to create specific slots visible in the front view.
To begin constructing the 3D model, the narrator starts with a sketch on the front plane and establishes the origin at the bottom center point for all measurements. Rather than drawing individual arcs directly, which can be difficult to manage regarding tangents, the strategy involves drawing full circles first and then trimming them later. The user adds an infinite vertical construction line as the axis of revolution and places five distinct circles representing different parts of the bishop: the neck, scarf, head, hat base, and the ball on top. Dimensions are carefully applied based on a provided engineering drawing; for instance, the outermost diameter is converted to a radius by halving it in SolidWorks, while other features like the scarf and head have specific radii defined relative to the origin or intersection points of previous circles.
A significant portion of the tutorial focuses on handling geometric constraints when creating the slot cut required by the design. The narrator encounters an issue where defining concentricity between new arcs causes alignment conflicts with existing dimensions, leading to broken geometry that does not sit perfectly vertically aligned as intended. To resolve this convoluted problem without over-constraining the sketch, a point is created at the intersection of two circles representing the hat and head sections. By making this specific point coincident with both circle centers, the user ensures perfect alignment while maintaining flexibility in positioning. After fully defining all dimensions for the cut profile using parallel lines and 45-degree angles, extraneous geometry is trimmed away to leave a clean region ready for an "extruded cut" feature that removes material through all sides of the part.
Once the sketch regions are prepared with no stray lines confusing SolidWorks about which area to modify, the revolution feature generates the main body of the bishop, resulting in a recognizable shape despite its unconventional proportions compared to standard chess pieces. The subsequent extruded cut is applied using the "through-all" option to create the necessary slot on the front face, ensuring the final model matches the engineering drawing specifications exactly. After verifying that both the revolved base and the cut feature align correctly with the original design intent, the narrator creates an isometric view of the completed part before exporting it, concluding a lesson that emphasizes using points and strategic trimming to manage complex constraints in CAD modeling.
Read the full video transcript
I'm going to be modeling this part which
is supposed to be a chess bishop and it
doesn't look like most Bishops because
most Bishops would have a longer top uh
maybe this is let's call this the head
just for agreed upon nomenclature here
the head of the bishop is normally
taller and uh stretched out a bit so if
I were to model this a little bit more
correctly I would use uh probably an
ellipsoid but for the purposes of this
being a relatively approachable example
it is a sphere
and this actually looks pretty
intimidating when you open it for the
first time you see lots of arcs lots of
Dimensions but when you get down to it
it's not that bad geometrically speaking
the main part of the bishop is actually
just like five arcs and a couple of
lines
so we're actually going to be modeling
this using two features the first
feature is going to be a revolution and
that'll be defined by a sketch
consisting of half of a cross section
from the front view and then we will
create a cut a linear cut from a sketch
on the front plane in order to match the
part that's shown here
so if I jump over to SolidWorks and
create a new part
I'm going to start with a sketch on the
front plane
now I'm going to arbitrarily decide that
the origin of my part will be the bottom
center
and then I will move all my lines
relative to that origin point so I will
start with the basic lines representing
the rough shape of the bishop
so I will add a horizontal line let's
try that again a horizontal line from
the origin
then a vertical line then a jut in and
then an angle line up
and I'm pretty much out of simple
straight lines
now I start venturing into Arc territory
and I personally think that in this
particular case it's actually easier to
draw whole circles instead of arcs and
then to trim off the parts that you
don't need trying to draw this is a
series of arcs just makes it a little
bit more complicated and it's harder to
recognize the patterns and kind of where
the tangents appear but before I launch
into Circle territory I'm going to add
my Axis of Revolution just to make it a
little bit easier to kind of visualize
what it's going to look like so I will
add a construction line of infinite
vertical height
starting from the origin
there we go
now I have my axis of Revolution I'll
add some circles so there will be one
Circle representing this surface one
Circle representing the uh I don't know
if this is the the head of the bishop
this is the Hat of the bishop
this is the scarf of the bishop this is
the neck of the bishop okay are we all
in agreement on that
so one of these circles will represent
the neck of the bishop one of the
circles will represent the scarf one of
them will represent the head one of them
will represent the Hat one of them will
represent the ball on the end of the Hat
I guess so I need five total circles
so I'll use the circle tool starting
from the center
and I will make one
and then two
and then what three ish
and then four and then
five
so I've recognized that these two
circles
are probably going to be coincident with
this center point of that Circle so I've
drawn it that way but the dimensions
will show us whether we're right or
wrong so we can get rid of that
coincident if we have to but let's begin
with those now I will start to Dimension
and I'm going to start like I drew I'm
going to start dimensioning from the
bottom center so I need to know this
distance here first
and the way that I do that is by looking
at this very scary looking top view
there are a lot of diameters given here
the relevant one here is the outermost
object line that has a diameter of 1.35
inches which is a number that I won't
remember for long enough to actually
make it into SolidWorks if you look at
the bottom of the front view here you
see how this point is vertically aligned
with these two points so that diameter
of the outermost object line could
represent this distance here this
distance here
or this distance here
so that was 1.35 oh yeah 1.35
so I'm establishing a radius instead of
a diameter so I will use half of 1.35
which I will allow SolidWorks to do that
math for me
and then I can't add a vertical distance
of this yet I'm going to leave that for
a little bit later
I know that you're probably concerned
because you can't see that on the front
view but that will that'll fix itself
later on we'll come back to that I swear
then I'm going to add the angle here of
45 degrees
and I will furthermore make sure that
SolidWorks knows these two lines should
be vertical from one another
cool and I double click to exit my
sketch for no reason particular I'm
going to jump back into it
and now I will add dimensions for this
circle
the center of that Circle
is vertically 1.3 inches away from the
origin so I will use the smart Dimension
tool and if you noticed when I was
diminishing that angle smart Dimension
is like its name would suggest pretty
smart so if I click on two lines it'll
try to figure out what dimension I'm
referring to and so if I click on the
center of this circle and then the
center of this origin depending on where
I move my cursor I can Dimension a
couple of things
so I could Dimension off this line if I
wanted to but I'm doing it for the
origin uh just for the sake of
demonstration so from the origin if I
drag my cursor over here to the right I
get a vertical distance so that should
be 1.3 inches
and then if I click on those two points
again
I can add a horizontal distance
which is shown on the side view of 1.7
inches
now I'll add a radius
it's shown as 1.5 I think SolidWorks
will make me Dimension a diameter so
that would be 1.5 times 2 which on most
days is 3
and I wow how did that end up being
let's try it again 1.5 times 2 is 3 not
4.5 there we go that neck is looking
right
so next up is the scarf I believe
let me drag my circle down to where I
expect it to be just to make that a
little bit easier that scarf has a
radius of 0.1 inches so a diameter of
0.2 inches
wow that's pretty close good eyeballing
me
and then the head of the bishop is not a
radius of 0.05 that would be this circle
down here in the cut
so I need to jump back up to the scary
top view and I recognize that the head
of the bishop is going to appear as an
object line from the top perspective
this bishop will have object lines here
here
I mean at the cut and then here
so in this case it's going to be the
object line that appears second from the
outside that's going to be the relevant
diameter
so second object line from the outside
from the outside from the outside is a
radius of 0.5 awesome so a diameter of
one I think
they're going five times two yes one
inch
and then I'm going to give this a radius
which of course is shown on the front
view that has a radius the Hat the base
of the hat or whatever is 0.5 so that
Dimension is going to be a diameter of
also 0.5 times 2 which I think is still
one and it is indeed still one
cool beans lastly the ball on the tip of
the hat which
is shown in the top view and this is
again going to be an object line and
this is going to be the smallest object
line as visible from the top so the
smallest object line is a diameter of
0.28125
nice round number
0.28125
0.28125 there we go cool now I have my
diameters my circles and this one is
positioned uh so I can start to position
the rest of them
so the first thing I'm going to do just
for my own sanity is get rid of this
coincident because that's one that I'm
kind of predicting so I don't want to
bind myself to it I want to make sure
that it's free to move around and then
if I think that it's coincident I can
add that back later if I need to but I
actually think that SolidWorks
and geometrically speaking this bishop
should end up pretty good so that is
going to be a height of 1.85 and that's
going to be this distance here
that's 1.85
and then the next circle is vertically
2.25 up so
2.25
and look at that look at that on the
circle
pretty much centered pretty close not
bad
good job geometry and then
my hat is tangent and the hat is also
going to be tangent to the axis
of Revolution so I'll add that now
so I'm shift clicking the circle and the
axis of Revolution I'm adding the
tangent constraint now that one's fully
defined last but not least is the ball
on the end of the hat which is
vertically three inches up
now I notice that I may have been wrong
about that tangent so I was given a
dimension here that's 2.875 that's
referring to the intersection between
the ball at the top of the hat and the
base of the Hat
so that's going to supersede the
Assumption of tangent between the circle
and the center line so I'll get rid of
that tangent and do this properly smart
Dimension origin
this intersection here
so that I'm going to have to do a little
bit differently I'm going to have to
clarify that I I'm defining a new point
and I'm going to tell SolidWorks that
there is a point at the intersection of
those two circles so I create a point
and then I draw a point and for the sake
of demonstration I'm going to draw that
point out here in space I now have a
point
now if I shift-click that point and this
circle and I tell it to be coincident
then I shift-click that point in this
circle and I tell it to be coincident
now that point is on both circles
therefore it is at the intersection
so I can move that around and adjust the
position of that base of the Hat Thing
so I'm going to use Smart Dimension
click on that new Point click on the
origin
give that a dimension of 2.875
2.875 and look at that
pretty close to tangent but
for the sake of round numbers we're
using that distance
cool so now I have some fully positioned
circles
now I'm going to go use my trim tool to
get rid of the extraneous parts of the
circles and power trim is the easiest
way to do that power trim you just kind
of click and drag and any line that you
go across and your click and drag is
removed and SolidWorks tries to figure
out like the two intersections on either
side of where you clicked through and
then it removes the things between those
two intersections so if I click and drag
through this circle you'll notice it got
rid of that big part of that Circle the
reason that this little line is still
shown is because that's used for
dimensioning it's for showing the
diameter of three inches so like if I
exit my trim tool and move this around
you'll notice that line disappears
it's not a real line so I will carefully
use my trim tool and get rid of some
more lines say that line don't need that
and nope whoops a little too
heavy-handed let's try that again um
that line and that line and that line
and that line and
and these two lines
and then that line and then that line
and that line and that line and that
line there I got rid of all of my
extraneous lines you'll notice that I
also kind of broke a couple of my
constraints that's okay I can go back
and fix those so one of the constraints
is the fact that
I think this line doesn't know
yeah so I need to clarify
that position again
so now that it's able to be moved around
I'm going to clarify that this head
which is going to be coincident to this
point
and then I'm going to make this point
that's the center of the scarf also
coincident to this Arc so I've basically
restored the fact that these two circles
had once been touching
so by making it coincident making this
Center Point coincident I'm telling it
that this Center Point and this line
should touch and even though they don't
touch I mean they would if this line
were continued it intersects with the
function of that Arc
now I believe all of my lines are fully
constrained I have the basic part except
for this thing we talked about
I need to bring this back so I'm I'm
actually going to be giving this a
horizontal distance not a vertical
distance so you see I can drag this
around and uh if I give it a horizontal
distance that'll bind its vertical
distance as well that's actually shown I
believe in two places on the top view
you can see that's the second line I
think yeah 1.25 it's also shown down
here for a little bit of uh over
dimensioning so 0.625 radius or a
point or 1.25 inch diameter so I'll use
this distance 0.625
all smart Dimension from the origin
again and then this point and I'll drag
it down to give it a horizontal
Dimension and that was 0. let's try it
again
0.625 inches
now I believe I have a fully constrained
sketch
so for good practice I will add a line
down the center to close the region
now with Much Ado I can create my
revolved base
and look at that I've got a good looking
Bishop
so if you just tried that at home and
you were unable to get it to work in a
single click like I just did you may
have had to go in and close your sketch
somewhere you may not you may have had
too many lines
um SolidWorks needs to know what the
region is that you want to actually
extrude the thing that you want to make
into a solid if if you had too many
lines you had may have had to go in
click this box and then click that
region that's a thing you may have had
to do but because I got rid of all of
the extraneous lines SolidWorks knows
the region that I want to extrude so
that was an advantage of doing it the
way that I did but regardless we have
the shape of our Bishop it's not a good
looking Bishop
I agree it is indeed now I'll add my cut
so I need that cut this slot to be
visible directly from the front view
which means I'm going to going to be
drawing on the front plane and then
extruding the cut
so I will create that basic shape on a
sketch on the front view again
so I will go up to sketch create a new
sketch select the front plane and now I
recognize that I begin with a circle
again and that Circle shares the same
Center Point as the head of the bishop
so if I kind of hover over this Arc
you'll see that nothing appears
isn't that nice so I will just add a
circle in the center arbitrarily and
then highlight the circle and the arc
out here
and then tell SolidWorks I want those to
be concentric circles so concentric
means sharing the same Center Point
and uh
that should be good
you'll notice that if I vertically align
it here that breaks and that's because I
actually in my original sketch yeah I
know saw it works it's a broken
Dimension it's fine
trying to prove a point you'll notice
that because I told SolidWorks to have
this Arc intersect at this point that
the center of that Arc isn't exactly
over the vertical point so the center of
that Arc according to the dimensions in
the drawing is not above the origin it's
not vertically aligned so this isn't
actually a sphere it's a slightly wider
sphere
foreign
going with concentric circles here is uh
not actually the best way to do that
because I mean if I were to Let's jump
back to the other sketch
I know it's still broken I'm trying to
prove a point SolidWorks give me a break
okay so by defining it to be concentric
with this Arc I am now not concentric
with this Arc so I have the option of
being either concentric with this Arc or
this Arc but not both and neither one of
those is going to be vertically aligned
so let's approach this from another
angle maybe instead of being
uh concentric to one of those maybe it
would be better to be centered on the
head of the bishop
to
say well if I want this to be vertically
aligned you'll notice that it didn't
break anymore and maybe
I want it to be positioned such that the
center of the arc or the center of the
circle here is vertically aligned
between these two lines all right
something like that or better yet I'm
actually going to use
um
a point again
if I use a Point again
I'm going to tell
the SolidWorks that this Arc and this
point
should be concentric
so by highly highlighting that point and
shift clicking this Arc out here I've
told SolidWorks to create a point at the
center of that Circle
now if I repeat that process
again I'm adding an arbitrary point I'm
highlighting this Arc out here
shift clicking this point
making them be concentric now I have two
points representing the center of both
of those arcs
so now if I were to add a construction
line between the two
I can add
this point which is the center of the
circle that I'm creating
and I can shift-click this line and make
that be midpoint
and that is the best way to Center that
Circle
how's that for convoluted it would have
been much easier to have interpreted the
engineering drawing as having
this be centered over the line and then
not having this line coincident to that
point
let's jump back to the other sketch here
I have a circle now completely The
Logical Circle I'm going to add some
lines because
circle plus some lines is the shape of
this slot that I want to cut so I'm
going to add some lines out here I'm
going to add a construction line
and put it from this point right here
too many points too close
and then I'm going to tell SolidWorks to
make these three lines parallel
let's try again these three lines
parallel
and then I'm going to Dimension this
line
and this
as having an angle of 45 degrees why
that surface you ask because that was
what was shown in the drawing
and then I am going to
have to close off this sketch in order
to create the cut so I'm going to add
another Arc here
and in this case I'm actually going to
use an arc instead of a circle so I'm
using a Center Point Arc and then I'm
using the center of this Arc over here
which again is represented by this point
and then I'm connecting these two points
here
so you know what just for
demonstration I'll just make this Arc
out in space I'll highlight this Arc and
then highlight this Arc make them be
concentric with it which they already
are and correadial
make this point and this line
coincidence
and that should result in these two
being pretty much coincident but I'll
add the constraint just for good measure
now that I have an arc completing the
sketch I can
trim off this extra bit of line
and then trim off this extra bit of
circle
now I'm going to add a diameter of the
circle which we can finally use this
radius here 0.05 inches
0 5
for a radius and now I have a fully
defined sketch with which to cut so I'll
exit my sketch I'll go to Features I'll
do an extruded cut
and I want it to cut all the way through
in both directions so I use the through
all
I click ok
and now I have my shape
so if I look at it from the front
that matches my drawing pretty well
so I I'm going to create an isometric
View and then export my part